February 2, 2022 at 1:43 amTomCSubscriber
I am trying to use ANSYS's fracture package to solve a fatigue crack growth problem - a fairly simple one for now. The model is a fairly standard notched tensile sample geometry with isotropic linear-elastic aluminum. I am using a Pre-meshed Crack object in the analysis. So far, I have encountered 2 issues.
- Solving the problem with just the Pre-meshed Crack defined gives me an incorrect answer for K1 (the primary stress intensity factor mode). It is a simple geometry, so I have a good analytical answer to compare. It is off by an order of magnitude. The stress in the part is correct; I don't know why the SIF isn't. It seems insensitive to mesh refinement.
- If I add a SMART Crack Growth object and set the Crack Growth Option to 'Fatigue', the solver crashes when reaches the "Calculating Fracture results" step. The error message in the Solver Output reads "For Cgrow Id 1 and Crack Id 1, the computed number of cycles is less than 1. Under this loading condition, static crack growth is expected. Please check your model, boundary conditions, and fatigue parameters. The crack growth solve is stopped." To thicken the plot, if I set Crack Growth Option to 'Static', the crack extension probe shows zero crack growth, and the SIFS (K1) result now returns the correct answer that it didn't return in 1.
My questions are:
- Any insight as to why I am not getting a correct SIF result without the SMART Crack Growth object?
- What might be causing the error message when I try to run the fatigue model? I'm relatively confident in my Paris Law coefficients, but I can't think of what else it could be and the error message hasn't changed despite trying a wide range of values.
- Are there any good resources floating around, especially working models with the SMART Crack Growth object? This site and Youtube seem thin.
Thanks in advance for any help!February 3, 2022 at 2:37 pmDavid WeedAnsys Employee
For the premeshed crack definition, how is the local coordinate system situated? It should be on the open side of the crack (typically offset by a small amount from the crack front): https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v221/en/wb_sim/ds_crack_overview.html
For the Pre-Meshed Crack and Arbitrary Crack objects, the origin of the coordinate system must be located on the open side of the crack.
Also, be sure to check your unit system, especially in terms of Paris' Law parameters.
February 10, 2022 at 1:59 amTomCSubscriberBoth of those suggestions were very helpful. Thank you.
Offsetting the local coordinate system from the crack tip solved issue 1. I had defined the C.S. at the crack tip based on some third-party videos that seem to have been inaccurate.
I found an error in my Paris' Law parameters. When I corrected the units, the error message in 2. went away and the problem solved.
February 11, 2022 at 3:46 pmDavid WeedAnsys Employee,you're welcome and glad this helped!
February 16, 2022 at 9:51 amDeerajkumarParthipanSubscriberI am trying to simulate a crack propagation using SMART crack growth technique in ANSYS Mechanical. I also have the same issues that had.
Even though I defined the local co-ordinate system away from the crack tip, on the open side, I am not observing any change in the SIFS. The values of SIFS are way higher than it should be.
can you please tell me what parameters did you change in the Paris law coefficients, because no matter what I try to do, I am getting the same error as before for fatigue crack growth.
Thanks in advance for any help!!
March 27, 2022 at 10:00 pmTomCSubscriberParis' law as defined in ANSYS uses 2 coefficients. One is a material constant, m. The other is a rate term, C, which is a function of both material properties and loading conditions. Neither is grounded in physical reality; they come out of a best fit from crack growth rate data. That's somewhat important to keep in mind, because they can vary a lot depending on what specific data is being used, even for the same material.
All that said, I used some textbook values for m and C of 7075-T6 Aluminum in R=0.5 loading.
Reference units of [m,N]
m = 3.70 [unitless]
C = 4.2937e-33 [(m/cycle)/(Pa-sqrt(m))^m
Where I got tripped up was in converting the units for C. It was reported with units of MPa, and to convert it I needed to be dividing by (1e6)^3.7, which was something that I had missed on first pass.
July 29, 2022 at 3:09 amj.thadathil_vargheseSubscriber
Hi, this is something related to and continuous to the previous issues. So I was able to rectify the SIFS experimental and numerical values for my model by changing the coordinates at the crack edge. However, I am not able to Crack propagation tool now. It shows a question mark even after putting in all the details. Any idea why this would be the case? Thanks.Viewing 6 reply threads
Ansys Innovation Space
- You must be logged in to reply to this topic.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.Trending discussions
- Solver Pivot Warning in Beam Element Model
- Saving & sharing of Working project files in .wbpz format
- Understanding Force Convergence Solution Output
- User manual
- An Unknown error occurred during solution. Check the Solver Output…..
- What is the difference between bonded contact region and fixed joint
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- whether have the difference between using contact and target bodies
- Defining rigid body and contact
- Colors and Mesh Display
© 2023 Copyright ANSYS, Inc. All rights reserved.Ansys does not support the usage of unauthorized Ansys software. Please visit www.ansys.com to obtain an official distribution.